Isolate Changed Dimension Example (C#)

//------------------------------------------------------
// Preconditions: The specified drawing and part
// documents exist.
//
// Postconditions:
// 1. Opens the drawing document.
// 2. Sets the system option to display
//    changed dimensions in the color selected
//    for Tools > Options > System Options >
//    Colors > Color scheme settings >
//    Drawings, Changed dimensions.
// 3. Saves and closes the drawing document.
// 4. Opens the part document of the drawing document.
// 5. Changes a dimension.
// 6. Saves and closes the part document.
// 7. Opens the previously saved drawing document.
// 8. Examine the drawing document to verify that
//    the changed dimension is displayed in the
//    changed-dimension color. Place your cursor over
//    the dimension to see its previous value.
//-------------------------------------------------------
using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;
using System;

namespace IsolateChangedDimensionsDrawingDocCSharp.csproj
{
    partial class SolidWorksMacro
    {
        public void Main()
        {
            ModelDoc2 swModel = default(ModelDoc2);
            ModelDocExtension swModelDocExt = default(ModelDocExtension);
            DrawingDoc swDrawing = default(DrawingDoc);
            string fileName = null;
            string saveFileName = null;
            int errors = 0;
            int warnings = 0;
            bool status = false;

            // Open drawing document
            fileName = "C:\\Users\\Public\\Documents\\SOLIDWORKS\\SOLIDWORKS 2018\\samples\\tutorial\\api\\box.slddrw";
            swModel = (ModelDoc2)swApp.OpenDoc6(fileName, (int)swDocumentTypes_e.swDocDRAWING, (int)swOpenDocOptions_e.swOpenDocOptions_Silent, "", ref errors, ref warnings);

            // Isolate changed dimensions
            // Equivalent to selecting Tools > Options > System Options > Colors >
            // Use specified color for changed drawing dimensions on open
            swApp.SetUserPreferenceToggle((int)swUserPreferenceToggle_e.swUseChangedDimensions, true);
            swDrawing = (DrawingDoc)swModel;
            swDrawing.IsolateChangedDimensions();

            // Save drawing document to another name
            saveFileName = "C:\\Users\\Public\\Documents\\SOLIDWORKS\\SOLIDWORKS 2018\\samples\\tutorial\\api\\box_changed.slddrw";
            swModelDocExt = (ModelDocExtension)swModel.Extension;
            status = swModelDocExt.SaveAs(saveFileName, (int)swSaveAsVersion_e.swSaveAsCurrentVersion, (int)swSaveAsOptions_e.swSaveAsOptions_Silent, null, ref errors, ref warnings);
            swApp.CloseDoc(saveFileName);

            // Open the part document referenced by the drawing document,
            // change a dimension, and save the document
            fileName = "C:\\Users\\Public\\Documents\\SOLIDWORKS\\SOLIDWORKS 2018\\samples\\tutorial\\api\\box.sldprt";
            swModel = (ModelDoc2)swApp.OpenDoc6(fileName, (int)swDocumentTypes_e.swDocPART, (int)swOpenDocOptions_e.swOpenDocOptions_Silent, "", ref errors, ref warnings);
            swModelDocExt = (ModelDocExtension)swModel.Extension;
            status = swModelDocExt.SelectByID2("Sketch1", "SKETCH", 0, 0, 0, true, 0, null, 0);
            status = swModelDocExt.SelectByID2("D2@Sketch1@box.SLDPRT", "DIMENSION", -0.03613329319351, -0.02215939491444, 0.02938582119709, true, 0, null, 0);
            Dimension swDimension = default(Dimension);
            swDimension = (Dimension)swModel.Parameter("D2@Sketch1");
            swDimension.SystemValue = 0.185;
            swModel.ClearSelection2(true);
            status = swModel.EditRebuild3();
            status = swModel.Save3((int)swSaveAsOptions_e.swSaveAsOptions_Silent, ref errors, ref warnings);
            swApp.CloseDoc(fileName);

            // Open the previously saved drawing document
            // and place your cursor on the changed dimension,
            // which displays in the color specified for
            // changed dimensions, to see its previous value
            swModel = (ModelDoc2)swApp.OpenDoc6(saveFileName, (int)swDocumentTypes_e.swDocDRAWING, (int)swOpenDocOptions_e.swOpenDocOptions_Silent, "", ref errors, ref warnings);
        }


        /// <summary>
        /// The SldWorks swApp variable is pre-assigned for you.
        /// </summary>

        public SldWorks swApp;

    }
}